CNC Tooling

[MichaelBick]

My team is ordering its firct cnc mill, a haas TM-2P, and I'm not quite sure what tooling to get. So far this is my list with the different questions I have. I'm thinking of buying a large part of this from Lake Shore Carbide and Maritool:

1/8" - 3/4" End Mills

• Do I need both roughers and finishers? How are the combined roughing and finishing end mills from Lakeshore?
• Which is better: Lakeshore variable flute end mills for aluminum or Maritool aluminum high helix end mills?
• For the maritool high helix finishers, which is the best coating?
• Should I get corner radius end mills in addition to square end mills?
• Should I get reduced shank end mill or regular length? Both?

4-40, 6-32, 8-32, 10-32 Specialty Aluminum Taps from Maritool

• Is spiral flute or spiral point better?

Reamers

• Do I need to get reamers for each of our common bearing sizes, or is the TM-2P precise enough with a regular end mill?

Drill/Mills

• Is it better to giet idividual tools for counterskining, chamfering, and spot drilling?

Ball End Mills

• Lakeshore variable flute ball end mills for aluminum vs Maritool 3 flute high helix end mill for aluminum?

Face Mills

• Which seller is best?
• Should I get multiple types(i.e. 45 degree and shoulder)
• What diameter should I get?

Drills from maritool

• Should I get screw machine length in addition to regular?
• Is carbide worth it?
• Should I get the 3 flute drills from maritool?

[AdamHeard]

Cory McBride. He's your guy for this.

[MichaelBick]

Originally Posted by AdamHeard

Cory McBride. He's your guy for this.

I'm hoping he'll respond to this thread. hint hint

[Gray Adams]

Endmills: Where I worked we used 3 flute carbide endmills from MA Ford. Probably the 116 series. I'm sure they aren't cheap, but they lasted a *long* time when run properly. We often used different tools for roughing and finishing, but they weren't roughing tools. They were just more worn down from so much cutting we didn't trust them for finishing. For my team, I've suggested they buy the 3 flute Aluminum specific endmills from maritool. We've made great use of roughing bits on the team, but somehow we usually got away with not using them at work.

Taps: Roll taps were the best. We didn't always use them, and I'm not sure why sometimes we used other taps, but we had various types of every size. The roll taps left stronger threads and they never jammed up and broke because of chips like the spiral flute taps do (because they don't make chips).

Reamers: You're never going to get a better hole than if you ream it. Always ream precision holes if you can. Even on a brand new VF3, we reamed high tolerance holes.

We chamfered, countersunk, and did spot drilling with 1 tool. We actually had 3 different tools, but they were just different sizes (1/4", 3/8", 1/2")

Shell mills: I mostly used 90 degree with rectangular inserts, but I've heard very good things about 45 degree with octagonal inserts. Mostly used a 3" tool, but the machines also had 2" tools.

Drills: If you can, I'd suggest you just get the 115 piece set, and individually buy a bunch of extra #43, #36, #29, #21, and #7 drills. That would cover you for #4-40, #6-32, #8-32, #10-32, and 1/4-20. The other drills don't get used all that much, so if your budget is restrictive a smaller set wouldn't really cause many problems.

Everything above is what we most commonly used, but our tool crib was full of specialty tools of every type, finish, and size (except the one you needed).

I'm sure Cory is going to show up with plenty more advice, and probably more applicable to FRC usage.

FWIW, my years on the team we used HSS Niagara cutter bits. We also struggled with speeds, feeds, and most importantly, a huge lack of decent coolant. We broke an insane number of cutting tools. The few carbide bits we had tended to shatter and the HSS bits would get hot, chips wouldn't clear out, they would weld on to the tool, and then it would snap off. We broke expensive tools (donations) too. So I'd just recommend taking it a little slow at the very beginning before you start throwing $30 endmills in there.

[sanddrag]

Cory helped me get set up with some suggestions from Lakeshore and Maritool. It's quality stuff. PM me your e-mail address and I can send you a list of what we ordered. I'd recommend more ER collet holders than endmill holders. More versatile.

[Cory]

I will try to post more later, but I'm in the middle of a ton of projects/work right now.

My best recommendation is don't splurge. Buy the things you know you will use all the time and add the rest later (unless you have the money now and have to spend it all right now).

We purchased a ton of tooling when we got our machine in 07 and to this day about 40-50% of that initial purchase has gone untouched because we didn't know exactly what we'd be doing and what we should buy.

We got a bunch of ball end mills and roughing end mills in regular and extended lengths as well as 2 and 4 flute end mills in regular/extended. We have pretty much any size you'd need and any type, but they aren't good for what we do every day. We've pretty much turned over all our tooling so that nothing we use on a regular basis is comparable to any of the tooling we initially purchased.

I like Lakeshore for end mills. Never really have purchased from Maritool, since their end mills have been more geared towards ferrous machining until recently. Don't bother with the roughing/finishing combo. Your machine doesn't have enough power to take full advantage of either. We have 2 flute and 3 flute in 1/8" increments from 1/4" to 3/4", with the vast majority being 1/4" and 1/2". 2 flute for anything under 1/4". If you treat them nicely they will last forever-I've been using one 3 flute 3/4" end mill for 3 years and a 3 flute extended length 1/2" end mill for almost as long. Pretty much the only reason you'll ever need to replace an aluminum specific EM is because you either did something stupid and broke it, or you couldn't evacuate chips fast enough to keep it from loading up and snapping. They really don't wear out.

The only coatings worth looking at are Zirconium Nitride, Molybdenum Disulfide (Destiny Tools' "Stealth" coating. Really awesome for aluminum), Titanium Diboride, and Titanium Carbonitride (ok, but not great). Avoid Titanium Nitride, Titanium Aluminum Nitride, or Aluminum Titanium Nitride like the plague for non-ferrous applications. These will cause aluminum to gall on the tool.

If you are just learning I would probably recommend against purchasing the aluminum specific tools up front. It's hard to justify spending 50 bucks on a 1/2" endmill that you are guaranteed to break in short order when you could spend half as much for a tool that will get the job done a bit slower. Once you have some experience operating the machine and aren't making as many mistakes they're a worthy investment.

I also like latheinserts.com. We bought a lot of aluminum specific inserted tooling (and some Destiny end mills) for our lathe and CNC mill from them. The owner is very friendly and helpful with recommending tooling for a given application. His prices are also extremely good and he will never try to sell you something you don't need.

[MichaelBick]

Thanks everybody. You've helped me to narrow down what to buy by a lot. This is the updated list of tooling to buy with comments and remaining questions:

End Mills(from Lakeshore, current ones are uncoated carbide, once we learn to use the machine we will be getting the specialty aluminum ones):

1/4" - 3/4" 2 Flute End Mills Regular Length
1/4" - 3/4" 3 Flute End Mills Regular Length
1/8" 2 Flute End Mill Stub Length(I feel like the majority of work done with a 1/8" end mill is on plate that had a maximum thickness of 1/4". Should I get both this one and the an 1/8" 2 flute regular length?)
1/4" 2 Flute Ball Nose End Mill(for any strange shapes we might have to make)

• Should I get any extended length end mills?
• Should I get any corner radius end mills?

Reamers(Solid Carbide from Maritool):

.874" Reamer
.875" Reamer
1.124" Reamer(anybody have a supplier for these. I've checked multiple online places and have not found a place that sells them yet)
1.125" Reamer

Face Mills:

• Which seller is best?
• Should I get multiple types(i.e. 45 degree and shoulder)
• What diameter should I get?

Drills(All regular drills are high speed steel from Maritool. If we need tap drill sizes or longer clearance sizes we will throw them in a drill chuck):

#9 Screw Machine Length Drill(10-32 Close Fit)
#21 Screw Machine Length Drill(10-32 Tap)
#18 Screw Machine Length Drill(8-32 Close Fit)
#27 Screw Machine Length Drill(6-32 Close Fit)
#32 Screw Machine Length Drill(4-40 Close Fit)
#9 Jobber Length Drill(10-32 Close Fit)
1/2" 82 Degree Countersink Drill from Maritool

• Is high speed steel sufficient for FRC?
• I figured that the tolerances on a cnc would be sufficient for close fit. Should I get free fit sizes instead?
• Should we keep the tapping drill sizes ready in our tool crib too?
• I decided against the mill/drill(combo tool for spotting, chamfering, and countersinking). Is this a bad decision?
• Has anyone used the maritool aluminum specific 3 flute drills?

Taps(thread forming taps, from Maritool):

4-40, 6-32, 8-32, 10-32 Taps

• any other confirmations on thread forming being better than spiral flute?
• spiral flute?
• recommendations on specialty aluminum taps from Maritool?

[Cory]

Do you have a budget? It's hard to give recommendations in a vacuum.

I would recommend against buying anything over 1/2" in carbide until you are familiar with the machine. You'll just be throwing away money and $86 is not a small mistake. I'd probably start with 1/8" 3/16" 1/4" and 1/2". You could throw 3/8" in if you like, but it's not super necessary. There's really never any reason to have end mills above 1/4" in increments of less than 1/8 though, and usually 1/4 is a better interval.

Depending on what tool holders you get (not a good idea to use in a collet chuck, as the flutes on the second end will get clamped against the collet), Lakeshore's double end mills are a good investment and can save you about 33% on sizes 1/2" and under.

Extended length isn't necessary at the start. You'll figure out what you need it for and then you can buy it as needed (probably only will need 1/4" and 1/2").

Corner radius is always preferred if you don't need a square shoulder. The number one reason end mills go bad is the corners of the flutes chip and then the cutting edge gets destroyed. Corner radii help prevent this.

Carbide reamers are a waste of money for FRC purposes (Maritool doesn't even sell anything above .500 in carbide). Stick with HSS.

We don't bother reaming anything we CNC unless we want a precise slip fit. Press fit bores are just as easily achieved via circular interpolation. It's generally a good idea to have a healthy stock of reamers though.

This is pretty much the best face mill you can buy for aluminum (we have one). The problem is the inserts are extremely pricey, only give you 2 cutting edges, and cannot be used to cut anything but aluminum or plastic. That kit is a fantastic deal as you would pay $700 for the inserts and body normally.

I'd probably recommend this guy as it's dirt cheap, has a unbeatable warranty (destroy it, even while being an idiot, and the replacement is free), uses cheap inserts that can be indexed 4 times, and can take inserts for ferrous and non-ferrous materials (he only sells ferrous inserts but I'm certain he could find you non-ferrous ones). Your machine can't take a decent cut with anything over 2". 45 vs 90 only matters if you intend to cut to a shoulder with the face mill. 45 cuts better.

Maritool sells nothing but high quality stuff, but you want bright finish drills and the only standard drill bits he sells are black oxide. Aluminum has an affinity for black oxide and will stick to it. The parabolic drills are unnecessary. They won't work well in anything but aluminum and a standard 118* or 135* drill works just fine in Al. No need for anything but HSS either.

There's nothing wrong with the 82* countersink, but you'll need either a spot drill or a mill/drill to spot drill holes and chamfer any features that are not holes. Close vs free doesn't have much to do with the accuracy of the machine as compared to what it is you're assembling and how much slop you can afford (or how much you need to actually be able to put it together). We use free because #7 becomes a dual purpose drill.

Form taps are great but they're a fantastic way to get yourself in trouble if you don't fully understand how they work and the relationship between percent of thread profile, class of thread, and H-limits. Essentially you have to drill a larger hole than a cut tap uses, but that hole is not always the same size depending on what the H limit of the tap you buy is.It can also become problematic when you have a part that for one reason or another you can't or don't want to tap on the machine and you drill it for a form tap and then someone else hand taps them with a cut tap without realizing the difference. They're also only good for ductile materials (aluminum, low carbon steels, some stainless)

More important than the cutting tools you get, you need to get workholding and toolholding. These are a significant investment relative to the cost of cutting tools.

[James Tonthat]

You must spread some Reputation around before giving it to Cory again.

This is one of the best threads/posts I've seen on Chief in a long time.

[Andrew Remmers]

Originally Posted by James Tonthat

This is one of the best threads/posts I've seen on Chief in a long time.

Agreed saving this one!

[scottandme]

Don't forget about workholding and toolholders are Cory mentioned. Those are the big expenses up front. Bare minimum you want a step block kit and 1 or 2 good vises. Kurt is the standard, but we have two Glacern 615's (http://www.glacern.com/gpv_615) that have been great. About half the cost of the comparable Kurt (3600V), it gives you the ability to clamp the vise on it's side for tall parts. Jaw bolt pattern is the same as the Kurt's, so you can use any of the industry standard step jaws, v-jaws, soft jaws, etc.

Are you set for CAM software? That's the other big consideration for most teams. We use EdgeCAM since we use it in our PLTW classes, but MasterCAM is probably the most widely used package.

I don't see much use for any end mills over 1/2" - it puts a big load on the pull stud, and the TM machines don't have a ton of torque/HP to start with. Power output drops off at high spindle speeds you'll be using for aluminum. There are motor curve charts out there if you do a little googling. Peak torque for the TM-2 is at 1200RPM as per the Haas site. For frame rails, gearbox plates, and the like, there's really not a lot of need for a huge end mill.

Form taps are good for small threads (#4 & #6), but for bigger sizes I've never seen a big advantage. Spiral point taps (shoot the chips ahead of the tap) for through holes, spiral flute taps pull the chips up and out the flutes of the tap (for blind holes). Buy a bunch of the appropriate wire gauge pilot drills (#36,29,21,7) in short or stub length. We buy the "Heat-Resistant Cobalt Steel Short-Length Drill Bits" from McMaster (28765A57), Cobalt is unnecessary, but McMaster only has TiN and Black Oxide in short length HSS, and those are both bad for aluminum.

Get a mill/drill with a 90 degree tip. McMaster stocks those as well. They can do triple duty (drilling, spotting, and chamfering).

[craigboez]

Originally Posted by Cory

Corner radius is always preferred if you don't need a square shoulder. The number one reason end mills go bad is the corners of the flutes chip and then the cutting edge gets destroyed. Corner radii help prevent this.

I thought I'd revive this excellent thread from the dead. Getting ready to purchase some new tooling, and I see there are usually several options for the amount of corner radiusing. For example, Maritool offers .008, .015, .030, .060, and .090 radius options for a 1/2" endmill. Never having purchased one I'm not sure why to choose one over the other. I'm assuming that the biggest radius will lengthen tool life the most, and since we are mostly doing thru-cuts on everything the radius will never have an impact on the cut geometry. Anyone care to elaborate on this?

[Cory]

Originally Posted by craigboez

I thought I'd revive this excellent thread from the dead. Getting ready to purchase some new tooling, and I see there are usually several options for the amount of corner radiusing. For example, Maritool offers .008, .015, .030, .060, and .090 radius options for a 1/2" endmill. Never having purchased one I'm not sure why to choose one over the other. I'm assuming that the biggest radius will lengthen tool life the most, and since we are mostly doing thru-cuts on everything the radius will never have an impact on the cut geometry. Anyone care to elaborate on this?

You have it right. Larger radius will reduce the chances of edge chipping and increase tool life.

[mman1506]

Would you mind sharing some fixturing techniques Cory? Are team is trying to figure out the best way to mill gearbox side plates.

[eli2410]

Originally Posted by MICHAELABICK

My team is ordering its firct cnc mill, a haas TM-2P, and I'm not quite sure what tooling to get. So far this is my list with the different questions I have. I'm thinking of buying a large part of this from Lake Shore Carbide and Maritool:

1/8" - 3/4" End Mills

• Do I need both roughers and finishers? How are the combined roughing and finishing end mills from Lakeshore?
• Which is better: Lakeshore variable flute end mills for aluminum or Maritool aluminum high helix end mills?
• For the maritool high helix finishers, which is the best coating?
• Should I get corner radius end mills in addition to square end mills?
• Should I get reduced shank end mill or regular length? Both?....

Michael, my team has a Techno LC 4896 (I'm 90% sure this is the model). Last year, all of our metal work was cut on this machine, running it sometimes for around 12 hours straight. The stuff that you need, in my mind is:

• 1/8" End Mill Bit that can cut metal
• 1/4" End Mill Bit that can cut metal
• Vacuum table to hold material down flat
• Sacrifice Board
• Metal Screws and such to attach the material to the sacrifice board
• Coolant (we used mist coolant, not sure the brand or anything else. I can get back to you on that. I see that your Haas TM-2P is made for flood coolant)
• CAM software, we used Mastercam last year with success. Our new Computer Integrated Manufacturing teacher has switched us over to EdgeCAM, we'll see how that goes
• Someone with experience. If you get wood-cutting bits (1/8" and 1/4" are fine), which I would recommend getting for training, have someone use the machine all first semester as much as possible to learn it and learn some of the shortcuts and such on the machine

That last one is big, even though it doesn't sound like it. The more people you get to use it during the offseason and the more hours that you have people working it during the offseason, the more parts you will feel comfortable with being cut on it. Also, the more people you have on it, the more efficient your team can be in cutting on it, since one person could run the machine, and the others that can CAM will be making the tool paths.

If anyone has any more questions feel free to ask. I haven't read through the entire thread as of right now, but I'll try to get to it.